Manufacturing DevBlog

Search non- Ballooned Components

By Xiaodong Liang

Question
I try to write a program which looks for components that are not attached with a balloon in each drawing. How could I search for the them?

Solution
There is not a direct API, but you can collect all components that has balloon. And filter out the components that has not balloon from all referenced documents of the drawing.

The VBA code assumes a drawing is opened with some balloons. It iterates each balloon of each sheet, get its referenced document. Finally, iterate each referenced document of the drawing, and filter out the documents that has not balloon.

Public Sub CreateBalloon()
   
    Dim oDrawDoc As DrawingDocument
    Set oDrawDoc = ThisApplication.ActiveDocument    
    Dim oSheet As Sheet
    Dim oBalloon As Balloon    

    ‘array to store the documents that have balloon 
    Dim oBolloonedDocs() As String
   
    Dim index As Integer
    index = 1

    
    For Each oSheet In oDrawDoc.Sheets
         For Each oBalloon In oSheet.Balloons
             Dim oBalloonValueSet As BalloonValueSet
                For Each oBalloonValueSet In  
                                 oBalloon.BalloonValueSets
                    Dim strDisplay As String
                    strDisplay = "Balloon Item Number: "
                   
                    ' Add the balloon item number
                            (the overridden value if there is one)
                    If oBalloonValueSet.OverrideValue = "" Then
                        strDisplay = strDisplay & oBalloonValueSet.value
                    Else
                        strDisplay = strDisplay &
                                     oBalloonValueSet.OverrideValue
                    End If
                   
                    Dim oDrawingBOMRow As DrawingBOMRow
                    Set oDrawingBOMRow =
                             oBalloonValueSet.ReferencedRow
                   
                    If oDrawingBOMRow.Custom Then
                        ' The referenced item is a custom parts list row.
                        strDisplay = strDisplay & vbNewLine &
                                      "Referenced Component(s):"
                        strDisplay = strDisplay & vbNewLine & "    
                                       Custom PartsList Row"
                    Else
                        Dim oBOMRow As BOMRow
                        Set oBOMRow = oDrawingBOMRow.BOMRow
                       
                        ' Add the Item Number from the model BOM.
                        strDisplay = strDisplay & vbNewLine & "BOM Item
                                       Number: " & oBOMRow.ItemNumber
                       
                        strDisplay = strDisplay & vbNewLine &
                                   "Referenced Component(s):"
                       
                        Dim oCompDefs As
                                ComponentDefinitionsEnumerator
                        Set oCompDefs =
                               oBOMRow.ComponentDefinitions
                          
                        If oDrawingBOMRow.Virtual Then
                            ' The referenced item is a virtual component.
                            strDisplay = strDisplay & vbNewLine & "     
                               Virtual: " & oCompDefs.Item(1).DisplayName
                        Else
                         
                            ' Add the document name of the referenced component.
                            ' There could be multiple if the balloon references
                            ' a merged BOM row in the model.
                            Dim oCompDef As ComponentDefinition
                            For Each oCompDef In oCompDefs
                                strDisplay = strDisplay & vbNewLine & "     " & oCompDef.Document.FullDocumentName
                                ReDim Preserve oBolloonedDocs(index)
                                oBolloonedDocs(index) = oCompDef.Document.FullDocumentName
                                index = index + 1
                            Next
                           
                        End If
                    End If
                    'MsgBox strDisplay
                Next
         Next
    Next
   
    ' check which document has not been ballooned
    Dim oDrawEachRefDoc As Document
     Dim oEachBalloonDoc As Variant
    
     Dim oStri_Unballooned As String
     oStri_Unballooned = "The document(s) that have not been ballooned" & vbCr
    
     Dim oIsB As Boolean
    
    For Each oDrawEachRefDoc In oDrawDoc.AllReferencedDocuments
   
       oIsB = False
       For Each oEachBalloonDoc In oBolloonedDocs
         If oDrawEachRefDoc.FullDocumentName = oEachBalloonDoc Then
            oIsB = True
            Exit For
         End If
        
       Next
      
       If oIsB = False Then
         oStri_Unballooned = oStri_Unballooned & oDrawEachRefDoc.FullDocumentName & vbCr
       End If
    Next
   
    Debug.Print oStri_Unballooned
End Sub

List Custom iProperties of selected occurrence

By Adam Nagy

As you can see in this blog post you can prompt the user to select an object using iLogic:
http://adndevblog.typepad.com/manufacturing/2013/11/do-selection-from-ilogic.html

Once you have the selected component then using the Inventor API you can also get all the iProperties from the document that is represented by that occurrence:
http://modthemachine.typepad.com/my_weblog/2010/02/accessing-iproperties.html

Here is an iLogic Rule that asks the user to select a component then lists its Custom iProperties: 

Dim entity = ThisApplication.CommandManager.Pick(
  SelectionFilterEnum.kAssemblyOccurrenceFilter, 
  "Select Component:")

If (Not entity Is Nothing) And _
(TypeOf entity Is ComponentOccurrence) Then
  Dim doc = entity.Definition.Document
  Dim propSet = doc.propertySets(
    "Inventor User Defined Properties")
  Dim msg As String
  For Each prop In propSet
    msg = msg + prop.Name + " = " + _
      prop.Value.ToString() + vbCrLf
  Next
  MessageBox.Show(msg, "iProperties")
End If

 If you want to do things wihtout the user having to select a component then you could do it like this:

Dim msg As String

' If you know the name of both the component 
' and the iProperties then you can do this
msg = "MyText = " + 
  iProperties.Value("TheBox:1", "Custom", "MyText")
MessageBox.Show(msg, "iProperties")

' If you only know the component name then
' first get the component
comp = Component.InventorComponent("TheBox:1")

' Then iterate through the Custom iProperties
Dim doc = comp.Definition.Document
Dim propSet = doc.propertySets(
  "Inventor User Defined Properties")

msg = ""
For Each prop In propSet
  msg = msg + prop.Name + " = " + _
    prop.Value.ToString() + vbCrLf
Next
MessageBox.Show(msg, "iProperties")

*.addin file version information

By Adam Nagy

The *.addin file that enables Inventor to find your AddIn dll and provides further information about it also specifies which Inventor versions the dll should be loaded into using one of the SupportedSoftwareVersionXxx tags.

The version info in the *.addin files follows the same logic that was used when the AddIn's still had to be listed in the registry. Here is some information about that from an older Inventor API Help file:  

Add-In Versioning

Most Add-In's need to confine their use to specific versions of Inventor. For example, an Add-In that takes advantage of any of the new API features in Inventor 6 will not work in Inventor 5.3. Add-In versioning allows the Add-In writer to specify which versions of Inventor the Add-In will be loaded in.

The versioning information is specified in the registry as a value within the Settings key. The names of these String values can be one or more of the following:

• SupportedSoftwareVersionLessThan 
• SupportedSoftwareVersionGreaterThan 
• SupportedSoftwareVersionEqualTo 
• SupportedSoftwareVersionNotEqualTo

The string associated with this value defines the version number. You can specify version numbers using two different forms:
[Major].[Minor].[ServicePack] or [BuildIdentifier]

The following are all valid version numbers:

• "5.3.2" - Specifies 5.3 SP2 
• "6.." - Specifies any version of Inventor 6 
• "..2" - Specifies any service pack 2. (This isn't very useful but just demonstrates that any of the Major, Minor, or ServicePack numbers are optional. 
• "6077000" - Specifies build 6077.

The SupportedSoftwareVersionEqualTo and SupportedSoftwareVersionNotEqualTo values can support multiple version numbers by separating them by a semicolon. For example, SupportedSoftwareVersionEqualTo = "5.3.0;5.3.2" will only support 5.3 and 5.3 SP2).

Autodesk Exchange Apps Hackathon – Big Success

By Virupaksha Aithal

The Autodesk Exchange Apps Hackathon – Big Success event is over. On behalf of the Autodesk Developer Network (ADN) team I’d like to say a big “thank you” to all the publishers who has registered and submitted Apps to Autodesk exchange store. We have received more than 110 Apps as part of this event till date. Till september 30th, publishers can submit the Apps as part of this event.  Visit http://adndevblog.typepad.com/autocad/2014/08/an-online-event-with-an-opportunity-to-receive-up-to-us-100-per-app-published-and-win-one-of-eight-i.html

PackAndGo from C++

By Adam Nagy

The Inventor API Reference provides VB.NET and C# sample codes, and there is also a blog post on it, but here is now a C++ sample too.

I simply used the SimpleApprenticeExe sample project and added the following to it:

#import "DTPackAndGo.tlb" no_namespace named_guids \
    raw_dispinterfaces raw_method_prefix("") \
    high_method_prefix("Method")

void PackAndGoSample()
{
  HRESULT Result = NOERROR;
    
  CComPtr<IPackAndGoComponent> packAndGoComp;
  Result = packAndGoComp.CoCreateInstance(CLSID_PackAndGoComponent);

  CComPtr<IPackAndGo> packAndGo =
    packAndGoComp->MethodCreatePackAndGo(
      L"C:\\Temp\\Source\\Assembly1.iam", L"C:\\Temp\\Destination");

  // Set the design project. This defaults to the
  // current active project.
  packAndGo->ProjectFile = L"C:\\Temp\\Source\\Test.ipj";

  // Set the options
  packAndGo->SkipLibraries = true;
  packAndGo->SkipStyles = true;
  packAndGo->SkipTemplates = true;
  packAndGo->CollectWorkgroups = false;
  packAndGo->KeepFolderHierarchy = true;
  packAndGo->IncludeLinkedFiles = true;

  SAFEARRAY * refFiles = NULL;
  VARIANT refMissFiles;

  // Get the referenced files
  packAndGo->MethodSearchForReferencedFiles(
    &refFiles, &refMissFiles);
    
  // Add the referenced files for package
  packAndGo->MethodAddFilesToPackage(&refFiles);

  // Start the pack and go to create the package
  // OverrideExistingFiles = TRUE
  packAndGo->MethodCreatePackage(VARIANT_TRUE);
}

As pointed out in the other blog post as well, a program that uses Pack and Go must be the same bitness as the Inventor they’re running with. If you’re using 64-bit Inventor then the program must also be 64-bit.

So I had to change the Project settings of the SimpleApprenticeExe sample on my Windows 7 x64 machine to x64: Download SimpleApprenticeExe_PackAndGo

I'm also attaching the sample Inventor 2015 project and document files that can be unpacked into the C:\Temp folder to test this program with: Download Source

Positions available at Autodesk

By Adam Nagy

Just a note in case someone is interested in joining our team.

There are two positions available in China, which are posted already and so can be applied for online:
https://autodesk.taleo.net/careersection/adsk_gen/jobdetail.ftl?job=14WD15487 https://autodesk.taleo.net/careersection/adsk_gen/jobdetail.ftl?job=14WD16108

We also have positions available in North America for M&E, which are not posted yet. Please get in touch with Kevin (kevin.vandecar@autodesk.com) if you're interested in those. 

Autodesk Exchange Apps Hackathon – update

By Virupaksha Aithal

Since we began the registration for Autodesk Exchange Apps Hackathon event, we received 145 registrations till date. We have received 74 Apps as part of the event. There is less than 3 days to the event. if you have not registered yet, visit Autodesk® Exchange Apps Hackathon http://exchangeapphack.com/

Discussions and presentations during the Hackathon include:

• How to architect your app for Autodesk Exchange?
• Developing cloud applications round table discussion
• Sustainability apps
• AutoCAD APIs roundtable discussion
• Advanced Exchange features – copy protection, IPN notifications, monthly subscriptions, selling web services
• Revit APIs roundtable discussion
• Max and Maya APIs round table discussion
• Inventor APIs round table discussion

for timing visit http://exchangeapphack.com/agenda/

Fast Open (Skip All)

By Adam Nagy

When opening a drawing you have some options:

If you check the possible values of the Options argument of Documents.OpenWithOptions in the API Reference then you can find the one corresponding to "Skip all unresolved files" - it's named "SkipAllUnresolvedFiles"

You won't find the equivalent of "Fast Open (Skip All)" listed though. It seems it was left out accidentally, but only from the API Reference. It is implemented in the API and can be used. It's named "FastOpen"

Apprentice in side thread

By Adam Nagy

A developer was using Apprentice in his application in a side thread so that it does not block the UI. It was working fine apart from getting a "Catastrophic failure (Exception from HRESULT: 0x8000FFFF (E_UNEXPECTED))" error when trying to access the Thumbnail of the Inventor document:

I'd like to point out that Apprentice does not support multi-threading or accessing it from different threads - at least it was not designed or tested for it. However, we can make the code work by turning the Thread into an STA thread:

private void buttonThread_Click(object sender, EventArgs e)
{
  Thread t = new Thread(new ParameterizedThreadStart(
    Program.UseApprentice));

  // Make sure to set the apartment state BEFORE starting the thread
  // Some info about STA:
  // http://blogs.msdn.com/b/jfoscoding/archive/2005/04/07/406341.aspx
  t.SetApartmentState(ApartmentState.STA);
  t.Start(this);
}

Source code: https://github.com/adamenagy/MultithreadApprenticeForm

 

Select plane of given part occurrence

By Adam Nagy

If you want to select one of the planes of a component occurrence inside an assembly, then you first have to get the component definition of that occurrence in order to get to its work planes. Then you need to get the work plane's representaion (proxy) inside the assembly through the component occurrence object:
http://adndevblog.typepad.com/manufacturing/2013/07/occurrences-contexts-definitions-proxies.html

In this case we select the XY plane of the currently selected part component occurrence:

Sub SelectXyPlaneOfOccurrence()
    Dim doc As AssemblyDocument
    Set doc = ThisApplication.ActiveDocument
    
    ' Let's say the occurrence is already
    ' selected in the UI
    Dim occ As ComponentOccurrence
    Set occ = doc.SelectSet(1)
    
    ' Let's select the XY plane (3rd in the list)
    Dim pcd As PartComponentDefinition
    Set pcd = occ.Definition
    
    Dim wp As WorkPlane
    Set wp = pcd.WorkPlanes(3)
    
    ' Get its representation in the
    ' assembly
    Dim wpp As WorkPlaneProxy
    Call occ.CreateGeometryProxy(wp, wpp)
    
    ' Now select it
    Call doc.SelectSet.Select(wpp)
End Sub